Anchor agitator

[Anonymous]

Hi All,

Have anyone of you tried to simulate an anchor agitator in a tank?

Right now I'm stuglling with this kind of problem. In my system I'm trying to simulate anchor agitator in a tank filled with water. I have created rotating region and run the simulation using frozen rotor approach. I have some doubts about the rotating region size (diameter), generally anchors are close -clearance impellers and due to this fact there is a small gap between the anchor and tank wall and to make matters worse (from the computational point of view) in this gap there is also the rotating region (like in the picture). Due to this fact I have some doubts about my results. They look realistic but the convergence plots are strange.

Do you have any suggestions how to coupe with meshing the gap with rotating region included?

I would be thankful for any idea.

I'm using:

- k-eps turbulence model,

- 3 deg per time step,

- impeller speed 100/minute,

- intelligent solution is enabled,

- ADV 5,

- inner iterations: 10, time steps to run: 598, Transient solution mode,

- dimensions: RR diameter=285 mm, tank inner diameter=300mm, impeller diameter=270 mm

   RR high is allso smaller then inner high of the tank (RR do not tuch the inner surfaces of tank)

- 294519 Total Nodes, 279477 Fluid Nodes , 15042 Solid Nodes

1286097 Total Elements, 1185691 Fluid Elements , 100406 Solid Elements

 Pawel

[Jon.Wilde]

Looks good to me. As this is transient I wouldn't expect a flat line convergence, more of a repeating pattern.

I think you could get away with moving this more per timestep than 3 deg. I would also suggest running this out for longer, something like 10-20 revolutions.

Hope that helps.

Jon

[Anonymous]

Thank you for the answer, I'll change per time steps to 1 deg.

Could you also advise me how to get the radial velocity in a plane (rotated about 45 deg from the position of anchor) shown in the picture. There is no problem for me to read the Vy or Vx velocity using a plot but when the plane is at an angle of 45 deg to XZ or YZ plane it’s not so obvious. I've imported the values of Vy and divided them by cos(45) but it seems that its not so simple.

I would appreciate any kind of idea.

[Anonymous]

...and one more thing. In the "Result Quantities" I've enabled Turbulent kinetic energy and turbulent energy dissipation but the results are just a "single" color - without any areas with higher or lower values. The same situation in Turbulent kinetic energy and turbulent energy dissipation.

[Royce_adsk]

A few suggestions with this model. As this is a 2 bladed rotating device I typically suggest a 1-3° increment. This is because of secondary flows that develop between the blade that you don't typically see when you have lots of fins to control the flow between blades.

For inner iterations I would leave this at 1 (If you were doing a free surface simulation I would stick to no more than 3).  This will greatly reduce your solve time.

Regarding frozen rotor. I would ignore this and just use a standard setup for the analysis. I really have not seen much luck using this option, but if anyone in the community can comment here that would be great!

For the radial velocity, you'll have to come up with the component velocity and then calculate the resulting vector for the angle that you are looking for.  If you look at a plane aligned with a X,Y, or Z axis then this calcualtion is easier.

The TED and TKE values, it seems you have clipped the results so much that you aren't seeing results. Try probing the plane with the dynamic probe to get an understanding of the value on a surface and then adust the range of the legend.

[Anonymous]

Thank you for the answer! I'm getting closer to the good results 🙂

I'm using frozen rotor approach because when I run the simulation using standard setup the solver crushed after about 500-700 iterations.

Regarding the component velocity, could you closer me how to implement this approach? Maybe there is a tutorial dealing with this?

I think the TED and TKE problem it;s not a problem of the legend. Looking at the convergence plot and the table I've found that TED and TKE values do not change during the simulation. I've searched the internet and found the following information:

http://help.autodesk.com/view/SCDSE/2013/ENU/?caas=caas/sfdcarticles/sfdcarticles/Turbulence-terms-c...

Some sugestions?

Pawel